Mold Design

You create a mold using a sequence of integrated tools that control the mold creation process. You can use these mold tools to analyze and correct deficiencies with either SolidWorks or imported models of parts to be molded.

Mold tools span from initial analysis to creating the tooling split. The result of the tooling split is a multibody part containing separate bodies for the molded part, the core, and the cavity, plus other optional bodies such as side cores. The multibody part file maintains your design intent in one convenient location. Changes to the molded part are automatically reflected in the tooling bodies.

The process is as follows:

Draft Analysis

Examines the faces of the model for sufficient draft, to ensure that the part ejects properly from the tooling.

Verifies that you have draft on your model, based on the angle you specify.

Creates a parting line from which you create a parting surface. The Parting Lines tool includes the option to select an edge and have the system Propagate to all edges.

Shut-off Surfaces

Creates surface patches to close up through holes in the molded part.

Parting Surfaces

Extrude from the parting line to separate mold cavity from core. You can also use a parting surface to create an interlock surface. See Interlock Surface.

Ruled Surface

Adds draft to surfaces on imported models. You can also use the Ruled Surface tool to create an interlock surface.

Tooling Split

Creates the core and cavity bodies, based on the steps followed earlier.

You can save each tooling body into a separate part document by right-clicking the body in Solid Bodies and selecting Insert into New Part. Then insert the new parts into an assembly, where you can add other supporting hardware, create mates, and so on. The new parts have external references to the original model, so changes to the molded part are automatically reflected in the tooling parts in the assembly.

The Mold Tools toolbar also includes additional tools common to the mold process, such as Scale and Move Face, as well as surface modeling tools such as Planar Surface and Knit Surface.

Parting lines lie along the edge of the molded part, between the core and the cavity surfaces. They are used to create the parting surfaces, and to separate the surfaces. You create the parting lines after the model is scaled and proper draft is applied.

To cut a tooling block into two pieces, you need two complete surfaces (a core surface and a cavity surface) without any through holes. Shut-off surfaces close up the through holes. You create shut-off surfaces after you create the parting lines.

You can insert a tooling split to create the core and cavity blocks for a mold. To create a tooling split, the part must have at least three surface bodies in the Surface Bodies folder: a core surface body, a cavity surface body, and a parting surface body. You can create a mold from a tooling split for multiple parts, or for multiple instances of the same part.

The Undercut Analysis tool finds trapped areas in a model that cannot be ejected from the mold. These areas require a side core. When the main core and cavity are separated, the side core slides in a direction perpendicular to the motion of the main core and cavity, enabling the part to be ejected.

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

The search functionality within the web help is in a beta test phase and you may experience periodic delays or interruptions in its performance. These are the normal and ordinary features of a beta test and shall not under any circumstances give rise to any liability on the part of Dassault Systèmes SolidWorks Corporation or its licensors. The topics within the Web-based help are not beta topics; they document SOLIDWORKS 2013 SP05.

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.